Reply To: How to extract running loads and moments from SHELL181 elements in workbench?

[peteroznewman]

Nastran writes no output unless you specifically request it.  Ansys writes most of the output you generally want and you have to change the output request defaults to reduce the output if the result file gets too large.  One item not output by default are Nodal Forces, which you need for what you want.  Under Analysis Settings, Output Controls, set Nodal Forces to Yes and Solve.

Create a Coordinate System where the XY plane cuts through the model where you want to obtain nodal forces and moments. Right click on that Csys and Create Construction Surface. Drag and drop that Surface onto the Solution branch. A Force Reaction probe will be created for that surface. Select the body that was meshed.

Click on the Solution branch. In the ribbon, choose the Solution tab and see there is a Probe button, select Moment Reaction. The location is Surface and the Geometry is the body again. Moment reaction has additional settings for Orientation which is best set to the Coordinate System defined for the surface and Summation which is best set to the Orientation System rather than the default of Centroid of the body.

The Force and Moment Reactions at a construction surface is like the FreeBody tool in Femap. It sums all the forces and moments at nodes on one side of the surface.